How to make a wide cut?

Using Fusion360 CAM I’m cutting through a 10mm thick piece of aluminium with a 3mm cutter using a 2D contour profile. How can I make the cut wider than 3mm to allow clearance for the chips?

Haven’t used fusion 360 but I would create an offset vector of your profile 3.5~4mm outside
of where you want to cut and do a pocket cut instead of profile.

Exactly what I would do in Fusion 360.

2D Contour, set a step-over value under Roughing Passes.
(The 5mm value, here I am using a 6mm end mill)

The rough pass will offset 1mm then do a second pass with 0 offset.

@HaldorLonningdal, the advantage of using a pocket is the ability to use an adaptive clearing strategy.

Thanks. Both good options. I plan to test both the adaptive clearing and roughing passes options tomorrow.
Had a couple of broken bit disasters today (too fast, too deep) so hopefully Posty will bring me some new bits tomorrow ready for the tests :slightly_smiling_face:

Yeah. 2D Adaptive do require a wider pocket to be effective, something around 2x bit diameter. That means clearing out more material than a 2D Contour roughing operation. But then the 2D Contour passes twice per depth so it is a trade-off.

Keep in mind one can with 2D Adaptive use different feed rates for cutting motion and non-engagement movements.

What kind of bit/flutes/rpm/feed rate are we talking about?

1 Like

3mm 2 flute cutter
Spindle speed 24000rpm
Feedrate 2000mm/min
Ramp feedrate 333mm/min
Pass depth 0.5mm

I’ve now adjusted this to a feedrate of 1000mm/min and a ramp feedrate of 200mm/min

A typical chip thickness for a 3mm tool is 0.025mm / tooth / revolution. This is highly governed by machine rigidity.

24000rpm x 0.025mm = 600mm/minute feed rate (per tooth)
So ideally you could aim for 1200mm/min for a 2F tool at 24k RPM

Runout, tool deflection and vibration all add up and need to be deducted from the 0.025mm/tooth number, but is hard to quantify so trial and error is expected. 2000mm/min is too fast as you have found out.

0.5mm DoC is a starting point, if all goes well you can try 0.75mm / 1mm DoC with the same feed rate/rpm with 2D Adaptive.
Eventually machine rigidity (lack of) will manifest itself and you have found your maximum Material Removal Rate (MRR) capacity.

Here is an example I did on my DIY CNC (Not Xcarve) with same pocket, same cutting parameters but increasing DoC using 2D Adaptive. It coped well down to 4mm, anything deeper it started to deflect.


Very interesting, thanks. My feedrate and DoC was based on trial and error (a lot of error), so good to see I’m not a million miles away from the calculated value.
Do you use coolant when cutting aluminium?

Yes, I use a mister (air) mixed with a light touch of denatured alcohol as my machining bed is wood and dont like liquid much. Flood clearing/cooling is better but require a fluid containment system.

I have also used WD40 successfully, only downside is that it leave behind some oil residue, the alcohol does not.

Here is a crude video of mine, running a 6mm 1F in aluminum:
(900mm/min @17k RPM and 6mm WoC / 1mm DoC)